à Siemens Ag, 2002. All Rights Reserved Sinumerik 840D/840Di/810D Programming Guide Cycles (Pgz) – 11.02 Edition - Siemens SINUMERIK 840D Programming Manual

0
11.02
2. Detailed explanations
In the theoretical sections, you are provided with a
detailed description of the following:
What is the cycle used for?
What does the cycle do?
What is the sequence of operations?
What do the parameters do?
What else do you have to look out for?
The theoretical sections provide learning material for
the NC beginner. You should work through the
manual at least once to get an idea of the scope of
the functions and capability of your SINUMERIK
control.
3. From theory to practice
The programming example shows you how to
include the cycles in an operating sequence.
An application example of almost all the cycles is
provided after the theoretical section.
ã Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Cycles (PGZ) – 11.02 Edition
Structure of the manual
03.96
2
Explanation of parameters
RFP and RTP
Generally, the reference plane (RFP) and the
retraction plane (RTP) have different values. In the
cycle it is assumed that the retraction plane lies in
front of the reference plane. The distance between
the retraction plane and the final drilling depth is
therefore greater than the distance between the
reference plane and the final drilling depth.
SDIS
The safety clearance (SDIS) refers to the reference
plane. which is brought forward by the safety
clearance. The direction in which the safety
clearance is active is automatically determined by
the cycle.
DP and DPR
The drilling depth can be defined either absolute
(DP) or relative (DPR) to the reference plane.
If it is entered as an absolute value, the value is
traversed directly in the cycle.
Additional notes
If a value is entered both for the DP and the DPR,
the final drilling depth is derived from the DPR. If the
DPR deviates from the absolute depth programmed
via the DP, the message "Depth: Corresponds to
value for relative depth" is output in the dialog line.
 Siemens AG 1997 All rights reserved.
SINUMERIK 840D/810D/FM-NC Programming Guide, Cycles (PGZ) - 08.97 Edition.
2 Drilling cycles and drilling patterns
2.1 Drilling cycles
If the values for the reference plane and the
retraction plane are identical, a relative depth must
not be programmed. The error message
61101 "Reference plane incorrectly defined" is
output and the cycle is not executed. This error
message is also output if the retraction plane lies
behind the reference plane, i.e. the distance to the
final drilling depth is smaller.
Programming example
Drilling_centering
You can use this program to make 3 holes using the
drilling cycle CYCLE81, whereby this cycle is called
with different parameter settings. The drilling axis is
120
always the Z axis.
30
0
N10 G0 G90 F200 S300 M3 Specification of the technology values
N20 D3 T3 Z110 Traverse to retraction plane
N30 X40 Y120
Traverse to first drilling position
N40 CYCLE81 (110, 100, 2, 35) Cycle call with absolute final drilling
depth, safety clearance and incomplete
parameter list
N50 Y30 Traverse to next drilling position
N60 CYCLE81 (110, 102, , 35) Cycle call without safety clearance
N70 G0 G90 F180 S300 M03
Specification of the technology values
N80 X90 Traverse to next position
N90 CYCLE81 (110, 100, 2, , 65) Cycle call with relative final drilling depth
and safety clearance
N100 M30
End of program
2-38
SINUMERIK 840D/810D/FM-NC Programming Guide, Cycles (PGZ) - 08.97 Edition.
0
Preface
Drilling cycles and drilling patterns
2
2.1 Drilling cycles
Z
G1
G0
RTP
RFP+SDIS
RFP
X
DP=RFP-DPR
2-37
08.97 03.96 2
Y Y
A - B
A
X Z
B
40 90
35 100 108
 Siemens AG 1997 All rights reserved.
0-11